Unleash Configurations in Parts and Assemblies with Alibre Design.

Unleash Configurations in Parts and Assemblies with Alibre Design.

Alibre Design’s configuration tools make it easy to change and manage parts and assemblies on the fly.

A new feature now available in Alibre Design Professional and Expert 9 lets users create multiple configurations for parts and assemblies. This feature adds new functionality to the design process and makes parts and assemblies easier to manage. For example, you can have a single part file and create variations of this part by setting multiple configurations. Likewise, you can have an assembly with multiple configurations, including those of different parts. In one of my recent articles, I gave an overview of using configurations in a part. This month, I’ll quickly review part configurations and then show you how to use those configurations in an assembly.

Setting Part Configurations

Before we proceed, let’s take a look at the configuration options available in the Part workspace.

Feature Suppression lets you suppress features so that they appear in some configurations but not others.

Parameter Values gives you control over dimensions and other parameters available within the Equation Editor.

Part Data (General Properties) lets you have different values under File/Properties.

Color Properties lets you assign different colors to a configuration.

Reference Geometry Hiding lets you hide and unhide reference geometry such as planes, axes and points.

Active Section View lets you use the selective Section Views on different configurations.

Download the hex bolt file.

Once you have the bolt, you can start to create configurations. To create a new Configuration in the Part workspace, go to the Insert menu and select Configuration, or in the Design Explorer, right-click Configurations and select New Configuration. The New Configuration dialog box appears.

The New Configuration dialog box.

You can lock on or unlock all options. For this demonstration, choose Lock All and name this second configuration 1.25 threaded. Once you’ve created the second configuration, right-click the first configuration in Design Explorer and select Edit. Rename it 1.25 non-threaded and lock all the options. This step protects the first configuration from being modified so that any changes done to another one are not applied to the first one. Once you have locked the first configuration right-click the configuration, 1.25 threaded, in the Design Explorer and select Activate. You can also double-click a configuration to activate it. Next, create a thread on the bolt. The bolt should look similar to the one below.

A threaded hex bolt.

Finally, let’s create a third configuration by following the steps described above, and this time name the configuration 1.75 non-threaded. On the Copy From field select: 1.25 non-threaded and lock all the options, then click OK.

Make the new configuration Active and modify it so that its length is 1.75, and the bolt should look like below.

With the new configuration, the 1.75 non-threaded hex bolt should look like this.

Save your part by going to File/Save and name it Hex Bolt. To see the different configurations, double-click on each one to activate them. If you need help creating any of the above examples, you can find more information in Alibre’s tutorials. To learn more about configurations, look at Creating Design Configurations. To learn how to create threads, see the Create Helical Geometry tutorial.

After you’ve created a part with multiple configurations, let’s look at how to use these configurations on the same assembly.

Set Assembly Configurations
In the next section, we’re going to create a simple block like the one below. Save the block on your computer in the Repository or the Windows file system.

To begin, draw a simple block and save it.

Next, create a New Assembly and insert the block by selecting it from the Part/Subassembly dialog box. Then click once on the origin to place a copy of the block and click Finish. Next, insert four copies of the hex bolt by going to Insert/Part/Subassembly and following the same steps. The bolt will have the same configuration as the last configuration saved before you closed the part file.

Next, start a new assembly and bring in four copies of the bolt.

For this example, we’re going to constrain the bolts to the corners of the block. First move the bolts by selecting the Move tool from the Assembly workspace, then select a surface on a bolt and select one of the directional arrows to move it in that direction. Do the same for the other bolts; this step is just an example so you don’t have to move them precisely.

Once you’ve moved your bolts over the block near each corner, mate them with the surface of the block by using the Insert Assembly Constraint tool on the Assembly toolbar to the right.

After the assembly is set up, go ahead and create new Assembly Configurations. The assembly configurations dialog box is similar to the part configurations with the addition of the following options:

Part/Subassembly Configuration allows parts and subassemblies to use different configurations.

Part/Subassembly Suppression allows parts and subassemblies to be suppressed from a configuration.

Part/Subassembly Hiding allows parts and subassemblies to be hidden on a configuration.

Constraint Suppression/Position Make Flexible allows a configuration to suppress assembly constraints and make subassemblies flexible.

First right-click the first configuration in the Design Explorer and select Edit. Change the name to 1.75 non-threaded bolts and Lock all options. Next, create a new configuration using the methods previously described and name it 1.25 threaded bolts, then Lock all the options and check the Active checkbox. Click OK. You should now have two configurations.

The assembly with two configurations.

Next, expand each one of the hex bolts in the Design Explorer. You’ll see the three configurations that you created previously. For each bolt, double-click the 1.25 threaded configurations to activate it.

To see what each assembly looks like from the inside, go to View/Display/Wireframe. Also make sure that the Silhouette Edges are enabled in the same View/Display menu. To toggle back and forth between configurations, double-click each assembly configuration to activate it. It should look like the picture below.

The 1.75 non-threaded configuration.

The 1.25 threaded configuration.

Configurations are a powerful functionality tool that can enhance your design process. I’ll end with an image of a suspension model that further demonstrates the power of configurations. Until next time, look for me as the Alibre Assistant online in Alibre Design.

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